Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Copy Features between Parts

11 REPLIES 11
Reply
Message 1 of 12
rcobbjr
773 Views, 11 Replies

Copy Features between Parts

I am trying to create an assembly. I want to copy the small threaded holes and position of the holes from the face of the large part and copy them to the circular part. I want to establish a relationship so if the hole positions change on the larger part they will also change on the attached circular part. How can this be done? See attachment for clarity.

11 REPLIES 11
Message 2 of 12
SBix26
in reply to: rcobbjr

Two methods that occur to me:

 

1. Adaptive  Edit the circular part (double click on it, or right click and select Edit); start a sketch on the face where you want to place the holes; using the Project Geometry tool, select the threaded holes from the large part; toggle the hole centers to centerpoint style; exit sketch; create holes.  The circular part is now adaptive in the context of that assembly, and hole postions will move with changes to the large part.

 

2. Multi-body Solids  Open the large part; re-create the circular part there as a New Solid, and projecting whatever geometry is useful from the large solid to the circular solid; use the Manage tab > Layout panel > Make Components tool to create two parts from these two solids and (re)place them in your assembly.  Any changes to the master part will be reflected in the assembly and component parts.

 

I generally prefer the second method, as it tends to be quite a bit more robust.  Parts can be adaptive in only one assembly, and adaptivity can get messed up pretty easily.  You typically want to turn off adaptivity as soon as that part of your design is settled, because it requires processor resources, and may interfere with constraints.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

Message 3 of 12
japike
in reply to: rcobbjr

You could also start a new part and use the derived component tool to add geometry from an existing part to a new part.

Peace,
Jeff
Inventor 2022
Message 4 of 12
jletcher
in reply to: rcobbjr

And the best way is to make the holes adaptive.

 

1. Put holes in flange do not dimension them.

2. Place flange and locate in assembly

3. Double click on the flange to activate it in the assembly.

4. Right click on feature of the holes you wish to match to other unit.

5. Finish edit.

6. Mate adaptive holes  using insert or mate using center lines to holes in other unit.

 

Then when done you can turn the adaptive off on the part by right clicking on the part and turn of adaptive no need to turn off adaptive in the feature.

 

Never use projected geometry for method of adaptive it will slow the performance down and also have other issues.

Message 5 of 12
rcobbjr
in reply to: SBix26

I followed these instructions. I changed the position of the holes and it seemed to work. I tried to do it again and now it does not work. I used the adaptive option. When I did it the first time, it automatically put the adaptive symbol next to the part name and the feature in the project browser.  When I repeated the steps, it now is NOT putting the adaptive symbol. What am I doing wrong?

Message 6 of 12
jletcher
in reply to: rcobbjr

Is this the same assembly?

Message 7 of 12
rcobbjr
in reply to: jletcher

Yes it is the same assembly

Robert Cobb, Jr.
Message 8 of 12
jletcher
in reply to: rcobbjr

Did you do my method or the project method? Sorry should have ask..

Message 9 of 12
rcobbjr
in reply to: jletcher

I used the adaptive method projecting the geometry. I just applied the same
steps to another project and it worked fine. But for this particular
project it is not functioning as it supposed to. Maybe a setting I don't
know. Interesting to say the least.

--
Message 10 of 12
jletcher
in reply to: rcobbjr

That is a method I don't like....... Mine never fails good luck...

Message 11 of 12
rcobbjr
in reply to: jletcher

I will try your method on this to see if I have any success. I will let you
know.

--
Message 12 of 12
SBix26
in reply to: rcobbjr

Is it possible that you've got the same part placed in two different assemblies somehow?  Any given part can be adaptive in only one assembly at a time, so that could explain why this one doesn't work.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report